Loft tool

- [Instructor] The SOLIDWORKS Loft featureis definitely one of the more powerful toolsinside of the SOLIDWORKS arsenal.The first thing I need to dois to create two or more sketchesthat we're going to loft between.So you can see here, I already have one sketch,and I need to create another sketch up above this.So to do that, let's go ahead upto Reference Geometry and create a plane.As far as my first reference,I'm going to go ahead and choose somethingthat's directly above this top plane here,and I can just drag that up if you'd like toby clicking on the arrow or typing a value here.

So type in, let's say 2.0.It's going to go ahead and push that planedirectly up above there by two inches.Then go ahead and click on OK.Now on that plane, let's go aheadand start a brand new sketch,and I'm going to go ahead and draw a center rectangleright there at the origin and kind of just drag it out.Now the exact science doesn't really matter,but I want to get something that's going to lookfairly interesting when I create this lofted feature.Alright, there's my sketch.I'm going to go ahead and just leave itundefined for right now,and let's go ahead and exit out of that sketch.So now I have sketch number one,and I have sketch number two,and I'm going to create a loft between the two.

Now for clarity, I'm just going to go ahead and hidethis plane here, so I'm going to turn the little eyeball off.So hide that. Alright.So now I've got the two shapesI'm trying to create a loft between.They both have the same amount of endpoints,so you got four corners here,and you got four corners there.So everything should be pretty good.So the first thing I want to dois come here to the Lofted Boss or Base command.As far as my profiles, now I can choose 'emfrom the window here, but I generally preferto choose them, actually, from the tree.So I'm going to choose this shape hereto that shape there, and automatically,it creates a loft between the two shapes.

Now you also have the option for usingStart and End Constraints or Guide Curves,but we'll be getting into those thingsin a few more minutes.First things first, just go ahead and click on OK,and you can see the shape that we have.Now if you want to go back and edit that loft,you can either change the individual sketches themselves,so they change to the sketch right here.Go ahead and drag this out a little bit, maybe even bigger.The loft will automatically updateto whatever shape you have between the two sketches.If I go back the other direction, same scenario.So now you've got the couple differentoptions for creating that loft.

Now if you actually want to change the feature itself,you can change, for instance,these start and end constraints.You can say none or you can change itto the direction vector, or you can to Normal to Profile.So Normal to Profile will basicallygive this some kind of a power.So it's saying, "I'm coming directly normal"out of that sheet of paper."And this little arrow here, if I click on that,controls how much power that has over the loft.So you can see by adding some strength to it,it's going to push up first before it actually comes back down,and you can get some pretty wild shapes just by doing so.

So you can really just kind of adjustyour loft with these commands.Same thing over here with the End constraint.Click over here, I can say Normal to Profile,and then you can see it's kind of makingmore of an hourglass-type shape,and I can push that down as well,and you get more of an effector more power in that normal direction.You can adjust those numbers to get a lotof different shapes very quickly and easily.If you want to try to use the other one,which is a direction vector,you actually have to put a direction in.In this case here, I don't really have a direction.

I would have to create some type of a linein the direction I'd like to go inor just choose some other existing line.But in this case, I don't really have any line,but that's how you'd choose it.You'd pick a line going the directionyou'd want it to go into, versusjust using Normal to Profile,which would be going straight down or straight up.So those are the basic thingsfor creating this type of a loft feature.Go ahead and click on OK, and there's my shape.Alright, I'm going to switch over to my second example.In this case here, I've created a loft already,and it goes from basically a square at the bottom up tierto a six-sided shape at the top.

And you can see here, I've got a couple of extra lines:this line here and that line right there,and it looks a little bit funny because right now,you've got a four-sided shape at the bottom,and you have a six-sided shape on the top.And so SOLIDWORKS does not know how to connect the dots.So it started to break this surface hereinto two surfaces as well as this one over here,and that's not really very symmetrical.So it's better to go and give SOLIDWORKSthe exact same number of sides for creating lofts,and let me show you how to fix that.Let's go ahead and just delete the loft for right now.

Alright, now let's go over into the very first sketchand notice it's blue.So let's go ahead and take this edge hereand this edge over here, and let's go aheadand switch them over to construction.So For construction and For construction.Now what I want to do is just createa regular line on top of there,so I make a line from here down to here,and from here...I can actually snap to the midpoint if you'd like to.And up to here.So now I've defined that, now I want to make all those equal.

'Kay, so this line is the same length as that line.Same thing over here.So we've got, actually, a six-sided shape.Even though it still looks like a square,it's still made up of six endpoints.So you got an endpoint here, here,here, here, here and here.Now when I go back and create that loft feature,it knows to connect this dot to that dot.From this dot to that dot, and so on.So let's go ahead and choose that first sketchand the second one, and then go ahead and chooseLofted Boss or Base, and notice over here,it didn't actually do what we want it to do.

It's kind of still twisting a little bit,and that means we need to adjustthese little green markers at the end.So if I click on this marker here,I can drag it over to here,and now I'm connecting the right dots together.Alright, once everything looks the way it should,let's go ahead and click on the green check mark again,and now we have our finished shape.So it looks pretty solid.Alright, the last one I want to show youis this one over here, which is the 8.1.3.,and alright, now we've got three shapeswe're going to loft between.And you can actually have as many sketch profilesas you need to create a loft.

So in this case, we're going to go from this oneup here to this one and then to this one up here.So go up to Loft Base or Boss,let's go ahead and choose it from the tree.Sketch number one going to sketch number two.And notice it's twisting already.So we don't want that twist, let's go aheadand grab that little green dotand move it over to the other side.So now it's looking pretty good,and then let's go ahead in that very last one.And again, it's twisting again,so we have to kind of move that around to the other side,so we start getting a better shape.Sometimes it has a kind of free-floating shape,so you can adjust it on the fly here,but right there, you can see we've gota pretty close to what we want.

We got this all kind of going in a row,and you can go ahead and click onthe green check mark to get that final shape.So we can adjust each one of those sketchesto change the shape if you want to.You can also grab those little green dotsand move it around a little bitto get a little bit variation in your shape if you need to.My general recommendation though,is if you have a multi-sided object,make sure you have the same amount of sidesin all your individual shapes.That way you'll always get the best styleof loft right from the beginning.

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Author

Released

10/31/2018

SOLIDWORKS is 3D CAD software that can speed up your design process and make you more productive—enabling you to deliver innovative products to market faster. In this course, Gabriel Corbett teaches you the essential tools and techniques necessary to create parts, assemblies, and drawings efficiently in SOLIDWORKS.

First, see how to create two-dimensional sketches that become the foundation for 3D objects. Next, look at extruding and revolving 3D features; creating complex objects using the Sweep, Loft, and Surface tools; and modifying parts. Find out how to create uniform holes with the Hole Wizard, and explore more advanced modeling techniques using equations, mirroring, and pattern tools. Then review best practices for putting parts together in assemblies. Finally, get tips for creating detailed drawings, complete with an itemized bill of materials.

Along the way, Gabriel highlights new features from the 2019 release, including Sketch Ink, which enables pen and touch markup and model manipulation using gestures, and the updated project curve and slice tools.